CNC deep hole drilling: how long holes are actually made

• 1
  What makes a hole deep
• 2
  Gun drilling, BTA, and when each one fits
• 3
  Coolant pressure, pecking, and the parameters that matter
• 4
  Straightness, drift, and the limits of the process
• 5
  Material behavior at depth
• 6
  Choosing a method for a given hole

Depth is measured against diameter, not against millimeters. A Ø10 mm hole 60 mm deep has a depth-to-diameter ratio of 6:1. Most shops call anything past 10:1 a deep hole, and past 20:1 the process changes completely. The reason is chip evacuation, not the drill itself.

A standard twist drill pushes chips up the flutes while the flutes are also the only path for coolant to reach the tip. Once the hole is around 4 to 5 diameters deep, that path is crowded. Chips pack, heat builds at the margin, and the drill starts to walk. The hole drifts off axis even if the drill is sharp.

The fix is a tool that separates the two jobs. A gun drill feeds coolant through an internal channel to the cutting edge, and the chips leave through a V-shaped external flute. Fluid does the transport work. The drill body only has to hold direction.

That single change is why a gun drill can hold a straight bore at 30:1 or 40:1, while a twist drill will not. It also explains the cost gap. A gun drill needs a starter hole, a guide bushing, and high-pressure coolant. You cannot run one on a standard flood-coolant vertical mill and expect the same result.

Table of depth-to-diameter ratios and what each one asks of the shop.

• 1
  Up to 5:1Twist drill, standard peck cycle, flood coolant is enough.
• 2
  5:1 to 10:1Carbide drill, higher pressure, shorter pecks.
• 3
  10:1 to 20:1Gun drill or BTA, guide bushing, pressure above 40 bar.
• 4
  Beyond 20:1Dedicated deep hole machine, tool runout under 0.01 mm.

Two families cover most work. Single-flute gun drilling uses a carbide or HSS tip on a long shank, with coolant pushed through the tool at high pressure. It suits holes from about Ø1.5 mm to Ø40 mm and holds straightness well because the tool is supported by the hole it just made.

BTA (also called STS) reverses the flow. Coolant comes in around the outside of the tube and chips exit through the center. The tube is stiffer and larger, so BTA fits holes from roughly Ø20 mm upward and removes material faster. The trade-off is that it needs more coolant volume and a bigger machine envelope.

The choice usually comes down to diameter and quantity. A batch of 200 valve bodies with Ø8 mm oil passages is gun drilling work. A single Ø60 mm hydraulic cylinder bore at 25:1 is BTA or boring work.

A third path exists: drill undersize, then bore or ream to size. It is slower per part, but it needs no special tooling and it tolerates a wider range of setups. For one-off parts, that is often the right call.

Coolant pressure is the parameter most people underestimate. At 10:1 the pressure needs to be high enough to move chips out of a narrow annulus, not just to cool the tip. Below roughly 40 bar, chips tend to recirculate and score the bore wall.

Peck depth has to shrink as the hole gets deeper. A common starting point is one diameter per peck at 5:1, then half a diameter per peck past 15:1. Full retract between pecks clears the flutes. Dwell at the bottom of each peck lets the spindle catch up with the feed.

Speed and feed depend on material more than on depth. Aluminum 6061 and 7075 tolerate high surface speed. Stainless 316 and 17-4PH work-harden at the margin, so feed per revolution has to stay above a floor value to keep the edge cutting rather than rubbing. Titanium TC4 (Ti-6Al-4V) needs lower speed and generous coolant volume to control heat.

Tool runout is the quiet killer. If the drill tip runs out by more than about 0.01 mm, the hole will bell-mouth and drift. Check runout at the tip, not at the collet.

A short starter hole or a spot with a stub drill reduces the initial walk. On a Ø6 mm hole at 20:1, that one step often decides whether the exit is on center.

Straightness is not the same as diameter tolerance. A hole can be perfectly round and still exit 0.5 mm off where the drawing says it should. On a 300 mm deep bore, a drift of 0.1 mm per 100 mm is common on a good setup; tighter than that needs in-process probing or a reaming pass.

Wall thickness matters. If the hole runs close to an outside surface, the tool is pushed toward the thin side because the material there deflects more. Roughly three hole diameters of wall thickness on each side keeps the bore centered.

Exit burrs and breakout are the other practical limit. When the drill breaks through, the last few millimeters have no support and the edge tends to chip. A support plate or a sacrificial backing block solves it on parts that allow the setup.

Cross holes are a scheduling problem, not just a drilling problem. Drill the deep bore first, then the cross hole, and deburr the intersection by hand or with a controlled back-chamfer. Doing it in the other order leaves a burr inside a bore you cannot reach.

If the drawing asks for a bore deeper than 40:1 with a tight straightness callout, the honest answer is that it may need a dedicated deep hole machine or a two-sided operation rather than a single pass.

Aluminum is the easy case. Chips break cleanly, heat leaves with the chip, and coolant pressure can stay moderate. 6061 and 6082 are predictable. 7075 machines well but is more prone to a gummy edge on deep cuts if feed is too light.

Stainless steels behave differently. 303 is free-machining and forgiving. 304, 316 and 316L work-harden, so the tool must stay engaged. Any dwell where the edge rubs without cutting raises local hardness and the next pass cuts worse.

Steels like 4140 and 4340 drill well in the annealed or normalized state. Hardened 4340 above roughly 40 HRC needs carbide and a rigid setup, and the cost per hole rises.

Titanium and Inconel are the slow end. TC4 and Inconel 718 hold heat at the cutting edge, so surface speed drops and coolant volume goes up. Tool life per hole is shorter, and that shows up in the quoted price.

Plastics and composites add their own problem: chip evacuation is easy, but heat can melt or delaminate the bore wall. PEEK and carbon fiber parts usually need lower feed, sharper edges, and a backing plate to avoid push-out at the exit.